NX7.5 Modeling 2

[CAD2015]

Hi,
Plase, have a look at the attached NX model.
How could I create:
1 - The profile of the green faces? (Helix/Tube?.... Doesn't work, not deep enough!)
2 - The profile of the yellow faces? (Covert to Sheet Metal/Normal Cut....? Yellow faces must be perpendicular on the faces they lie on)

 

[cowski]

For the green faces, I'd try to sweep a rectangle along a helix and blend the result.

For the yellow faces, copy the outer circular face (extract face, with delete hole option) and extract the edges of the existing hole; trim the face to the extracted curves and thicken the resulting sheet. The thicken command will create faces perpendicular to the extracted face.

www.nxjournaling.com

 

[CAD2015]

cowski,
Thanks for your replay.
Sweep using Helix would create a profile perpendicular on the Helix curve on it's entire guide but angled on the face of the Cylinder (I tryed that, first).
The profile for Subtraction should be fully paralel to the face of the Cylinder........

 

[cowski]

Sweep using Helix would create a profile perpendicular on the Helix curve on it's entire guide but angled on the face of the Cylinder

Not necessarily, it depends on the creation options you use. I'd use the vector direction orientation option and choose the vector of the cylinder.

www.nxjournaling.com

 

[JohnRBaker]

OK, In the attached model, I've replaced one of the 'Yellow' sets of faces with a set of 'Cyan' faces, which are normal to the outer surface. Just look at what I did and you should be able to do the same with the other.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[CAD2015]

Thanks John and all that answered!
Another Star for you and for the people that reply to my thread!
How about my first question "(1 - The profile of the green faces)"?...........

 

[JohnRBaker]

Not sure what you mean by the 'profile'? Are you talking about a perpendicular cross-section through the 'bead'?

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[CAD2015]

I name "Profile" the feature that is colored in green.
Green faces mark the feature that I need to create........
I made those faces in green for better references.
I probably need a Subtraction, but I do not know what Tool should I use for accurate design (The part I attached to my Thread is a Body feature, it is not parameterized.
I need to create a parameterized part!

 

[Toost]

Here's an attempt. It is not truly identical, the helix is constructed based on the assumption that the bottom of the bead is a swept circle, i.e the center of this "circle" is the start point of the helix. ( It is no true circle due to that it is free form geometry.) I drew a little helper line across this "arc" and used the midpoint of this line. The line from that midpoint to the centerline has the purpose to set the origin of the helix. The pitch of the helix is also "assumed", then a sketch which mimics the "intersection curves" that a datum plane normal to the helix pproduces. The sketch is swept with orientation method "Vector" along the helix. Then the ends of the sweep is in my model far more abrupt than the original model. I did not focus on these. In the end i used the Sheet metal Solid Punch to apply the shape to the original body.

The cross section of my model is not identical to the supplied model, this might be because i have done erratic assumptions, but it might also be because the designer of the imported model made mistakes (!)

Regards,
Tomas

 

[CAD2015]

Thanks a lot, Toost!
A Star for you!